Helical Gear
 

 

In this tutorial you will learn how to create a helical gear. To do this tutorial you must first have completed the basic gear tutorial.

 

Start a new design

Set the Units to inches

Tools>Options>Units

Create the gear body on the base workplane, initial sketch.

  • Draw a circle of with a radius of 3"
  • Extrude, add, 2", symmetric OK

 

Start a new sketch on top of the gear body. Call the new sketch front tooth

  • Project the gear body circle into the sketch
  • Draw a vertical straight line from the center of the circle and toggle it to a construction line

 

 

  • Zoom in on where the vertical construction line intersects with the projected circle
  • Draw half of the tooth as shown
  • Make the slanted line go thru the gear body circle to avoid the automate tangency (with circle) constraint.
  • Trim off the excess line that comes thru the project circle

 

 

  • Mirror the half tooth about the veritical construction line.
  • Add a horizontal construction line that connects the bottoms of the tooth. This line will be used for dimensioning.

 

  • Dimension the tooth sketch as shown
  • To get the top tooth dimension click on the end point of one side then click and drag from the end point on the other side
  • Make sure your height dimension is from the construction line to the top of the tooth. NOT the length of the angled line.

 

Trim away the portion of the prohject circle that is not needed. This will leave just the front of the tooth as one completed sketch
This completes the front tooth sketch. We will be lofting this sketch to the rear tooth sketch.

 

To create the rear tooth sketch we will follow the above procedures but offset the tooth by 15 degrees

Select the rear gear body surface and start a new sketch. Call the new sketch rear tooth.

 

  • Project the gear body circle into the sketch.
  • Project the vertical construction line in the front tooth sketch and toggle it to a construction line.
  • Draw a construction line at an angle to the vertical construction line and give the angular offset a dimension of 15 degrees.

 

Create the rear tooth sketch as shown.

  • When you draw the top of the tooth make sure you add a perpendicular constraintbetween the line and the construction line.
  • Mirror the half of the tooth.
  • Add the construction line connecting the bottoms of the tooth.
  • Add the dimensions

 

Trim away the unneed parts of the projected circle. You will need to trim in two areas since the construction lines broke up the circle

 

We will now create the tooth feature

  • Feature>Loft Thru Profiles
  • With the line select tool, select a line on the front tooth sketch and a line on the rear tooth sketch.
  • Make sure the corners that the loft line stretch to are "matching" corners. More the yellow box (click-n-drag) to make it so.
  • OK

 

Now you will use the pattern command to create the rest of the teeth

Use the feature select tool to select the new tooth.

Feature>Pattern

Use the edge select tool to select the circle as the direction for the pattern

Make 15 instances

Angle of 360/15

OK

 

 

 

Complete the gear by projecting a 2.5" radius hole thru the gear body

 

 

 

  
Tutorial By Steve Schweitzer, 2001